Jump to content

Welcome to eMastercam

Register now to participate in the forums, access the download area, buy Mastercam training materials, post processors and more. This message will be removed once you have signed in.

Use your display name or email address to sign in:

prmcode


K2csq7
 Share

Recommended Posts

Ok, I stand corrected. The .Ops file went away in X3 or X4, the Parameters are now written to a "Memory Map". This is basically the same process as before (with the Ops file), but it is cleaner and doesn't involve using an 'external' file. Also, the Parameter Read/Write functionality was added to the MP Language by Jeff Hill, and Paul did the rd_cd, rd_md, stuff in the the Post file.

 

One thing about working here, it keeps you on your toes...

Link to comment
Share on other sites

Keith,

 

As Paul stated, there is no way to access those limit parameters. Those particular data fields are part of a package that CNC Software purchased from Module Works. Due to that fact, we can't write them to the memory map.

 

Tim,

 

I'm not sure what the old plans were, but the NCI file isn't going away, and the .ops file has changed. It is now part of the 'Memory Map', which is basically a chunk of Memory that temporarily holds all this information, and is discarded when the Posting process completes.

 

We do have changes coming to the NCI, but I can't really talk about that yet.

Link to comment
Share on other sites
As Paul stated, there is no way to access those limit parameters. Those particular data fields are part of a package that CNC Software purchased from Module Works. Due to that fact, we can't write them to the memory map.

 

Ya but you could copy those para's using some sort of hypertext protocol and capture the contents of those zones on the screen. All one would have to do is to pull up that axis menue to trigger it store to a buffer.

Link to comment
Share on other sites

Keith what was the "post work" you were wanting to do. Maybe there's another route to get there. Maybe set up min_limit_c and max_lim_c and in pcout/pfcout:

 

pcout/pfcout

if cabs < min_limit_c, min_limit_c = cabs

if cabs > max_limit_c, max_limit_c = cabs

 

If you needed it at top of nc you could write everything to subout = 1 then in peof switch to subout = 0 put limits in and mergesub?

 

 

Colin, I never noticed the .ops file wasn't there any more. Memory map is basically the same thing then, just available at run time?

Link to comment
Share on other sites

M30,

 

I'm glad you've taken an interest in editing Post Processors, but some of the information you posted is incorrect, so I'm going to take a minute and clear some of that up.

 

 

Much appreciated. There is always more to learn. Some of what I assume to know is empirical, and based on working with posts alone. I love hearing the straight facts from the source. It would be awesome if some of this information was stickied in a post processor section of the forum.

 

Good discussion all. I'm enjoying it.

 

Cheers,

 

M30

[email protected]

Link to comment
Share on other sites

prmcode$ 10120. 	0
prmcode$ 10121. 	0
prmcode$ 12258. 	0
prmcode$ 12259. 	0
prmcode$ 12260. 	0

 

Awesome Colin, thanks for not letting this one die...anyone have a clue as to why my "parameter dump" skips the parameters I need?

I read that these values would be output in radians instead of degrees...

Link to comment
Share on other sites

Me to M30, good stuff

 

Jimmy, what I am doing with this stuff is...My machines are not really full 5 axis (big horizontals with a rotary on a rotary) (the rotarys don't stop on a dime) so for rotary work I set the limits so the XYZ axes take care of the "ends" of the path and the rotary does all the stuff in the middle. When the machine is moving XYZ it takes the feedrate as a normal IPM feed, when the rotary is the only one moving the machine/control sees the feedrate as degrees per min.

I have added stuff to the post so when the machine is on the "limits" I set (pic in first post in this topic) it will change the feedrate to a different value (one I specified in the tool defintions' plunge rate), not the operations plunge rate (inches per min)) and when it is not on the limits the feedrate gets output as the operations feedrate (I plug it into the operation as degrees per min).

 

It is working great so far... here is what the posted code looks like..(surfacing toolpath stepping over in X). For the code below 24.8 is the feedrate in IPM and 83 is the degree per min equivalent. The finished surface does leave visual evidence of the feedrate transition, but no gouging. (You wouldn't see it if I didn't show you)

 

(  1/4 BALL ENDMILL   )
N204 M11 (UNLOCK 
N206 M21 (UNLOCK C)
( LOAD T2 M06 )
N208 M00
( CONFIRM T2 H2 D2 DIA =.25 TOOL OAL: 2.5 )
N210 G0 G17 G90 G54 X-41.5603 Y-6.6474 C12.952 B75.28 S1400 M3
N212 G43 H2 Z-12.5517
N214 X-35.1868 Z-14.2261
N216 Z-14.6261
N218 G1 Z-15.0261 F24.8
N220 X-35.1729 Y-6.5068 Z-14.9732
N222 X-35.1588 Y-6.3602 Z-14.9194
N224 X-35.1455 Y-6.2187 Z-14.8688
N226 X-35.1441 Y-6.2034 Z-14.8634 C13.391
N228 C13.868 F83.
N230 C14.353
N232 C14.83
N234 C15.309
N236 C15.785
N238 C16.259
N240 C16.734
N242 C17.203
N244 C17.676
N246 C18.142
N248 C18.613
N250 C19.074
N252 C19.544
N254 C20.
N256 C20.503
N258 C20.98
N260 C21.49
N262 C21.966
N264 C22.483
N266 C22.96
N268 C23.483
N270 C23.96
N272 C24.489
N274 C24.966
N276 C25.502
N278 C25.979
N280 C26.522
N282 C26.998
N284 C27.548
N286 X-35.1313 Y-6.0636 Z-14.8148 C27.555 F24.8
N288 X-35.1166 Y-5.898 Z-14.7588
N290 X-35.1043 Y-5.7551 Z-14.712
N292 X-35.0889 Y-5.7569 Z-14.7123
N294 X-35.1012 Y-5.8998 Z-14.7592
N296 X-35.1159 Y-6.0649 Z-14.815
N298 X-35.1286 Y-6.2047 Z-14.8636 C27.548
N300 C26.998 F83.
N302 C26.522
N304 C25.979
N306 C25.503
N308 C24.966

Link to comment
Share on other sites

If I understand correctly you want it to change feedrates if only a rotary axis is moving by itself.(?)

 

Maybe an easier way to do it would be to test xinc,yinc and zinc to see if any of those are moving. Maybe add something like this to pfr$

 

feed_chg : 0
pfr$
  feed_chg = 1
  if xinc <> 0, feed_chg = 0
  if yinc <> 0, feed_chg = 0
  if zinc <> 0, feed_chg = 0
  if feed_chg = 0, feed_out = fr_pos$
  if feed_chg = 1, feed_out = other_feedrate

Link to comment
Share on other sites

Join the conversation

You can post now and register later. If you have an account, sign in now to post with your account.

Guest
Reply to this topic...

×   Pasted as rich text.   Paste as plain text instead

  Only 75 emoji are allowed.

×   Your link has been automatically embedded.   Display as a link instead

×   Your previous content has been restored.   Clear editor

×   You cannot paste images directly. Upload or insert images from URL.

 Share

  • Recently Browsing   0 members

    • No registered users viewing this page.

Join us!

eMastercam - your online source for all things Mastercam.

Together, we are the strongest Mastercam community on the web with over 56,000 members, and our online store offers a wide selection of training materials for all applications and skill levels.

Follow us

×
×
  • Create New...